WCS vs Machine CS (Resolved)

[martyscncgarage]

Watching Keith's mill training video may help a little bit:


And read through the Mill Operator's Manual:
https://www.centroidcnc.com/centroid_di ... -v4.14.pdf

[cnckeith]

viewtopic.php?f=63&t=1801

[cnckeith]

martin,
hello. the travel exceeded message in the second video was for Z. this means that the program with the tool offset value will not fit on the machines base on the current Zwcs 0 position. so, you have any number of items not set right. 1.) wrong tool being called., 2.) correct tool but wrong offset, 3.) offset not set 4.) WCS z zero position not set correctly 5.) program asking for or a combination of all of them.

the line that issued the message has a Positive Z move of 15mm with tool height of H8.

Use F8 Graph to find out which lines are causing the travel exceeded message and then go track it down. zoom out to see all of the moves and observe the scale to determine distance etc..
I loaded the program provided 1001.nc and set a WCS x0y0z0 in the Middle of the machine work envelope.
and got x travel exceeded line 34, then i went to took a look at line 34.
here is the entire program
%
O01001
(T8 D=8. CR=0. - ZMIN=-1. - flat end mill)
G90 G94 G17
G21
G28 G91 Z0.
G90
(2D Contour1)
T8 M6
S3200 M3
G54
G0 X-37.365 Y26.344
G43 Z15. H8
Z5.
G1 Z1. F266.67
Z-0.2
G19 G2 Y25.544 Z-1. J-0.8 K0.
G1 Y24.744 F800.
G17 G3 X-36.565 Y23.944 I0.8 J0.
G1 X36.565
G2 X40.565 Y19.944 I0. J-4.
G1 Y-19.944
G2 X36.565 Y-23.944 I-4. J0.
G1 X-36.565
G2 X-40.565 Y-19.944 I0. J4.
G1 Y19.944
G2 X-36.565 Y23.944 I4. J0.
G3 X-35.765 Y24.744 I0. J0.8
G1 Y25.544
G19 G3 Y26.344 Z-0.2 J0. K0.8
G0 Z15.
G17
G28 G91 Z0.
G28 X0. Y0.
M30
%

the cad/cam system you are using needs some work in the post processor department. line 34 (in red) shouldn't be there and is causing issues.
i deleted it and the program graphs and runs fine with your report.zip configuration settings loaded on my machine

[cnckeith]

i created a very similar part program in Intercon so you can see what the G code should look like.

; ICN_PATH = C:\intercon\martin.icn
; --- Header ---
N0001 ; CNC code generated by Intercon v4.49 BETA, Rev 1
; Description: rectangle
; Programmer: martin
; Date: 12-Feb-2020
M25 G49 ; Goto Z home, cancel tool length offset
G17 G40 ; Setup for XY plane, no cutter comp
G21 ; millimeter measurements
G80 ; Cancel canned cycles
G90 ; absolute positioning
G98 ; canned cycle initial point return
; --- Tool #8 ---
;Tool Diameter = 8.0000 Spindle Speed = 3200
;
G49 H0 M25
G0 X0.0 Y0.0
N0002 T8 M6
S3200 M3
G4 P3.00 ; pause for dwell
G43 D8
; --- Frame (Outside Rect) ---
N0003 X36.365 Y27.94 Z2.54 H8
G1 G91 X0.0 Y0.0 Z-2.54 F50.0
X0.0 Y0.0 Z0.0 F266.0
X0.2 Y0.0 Z-0.2 F50.0
X-73.13 Y0.0 Z0.0 F266.0
G3 X-8.0 Y-8.0 Z0.0 J-8.0
G1 X0.0 Y-39.88 Z0.0
G3 X8.0 Y-8.0 Z0.0 I8.0
G1 X73.13 Y0.0 Z0.0
G3 X8.0 Y8.0 Z0.0 J8.0
G1 X0.0 Y39.88 Z0.0
G3 X-8.0 Y8.0 Z0.0 I-8.0
G0 G90 X36.565 Y27.94 Z2.54
; --- End of Program ---
N0004 G49 H0 M25
G40 ; Cutter Comp Off
M5 ; Spindle Off
M9 ; Coolant Off
G80 ; Cancel canned cycles
M30 ; End of program

[cnckeith]

[Martin Zarnay]

Hi guys
Thank you for all your suggestions, I will take a look at steps in ( Y 6402 ), and suggestions about Z height. But my problem was about X travel, and I have to say that it is solved. I hope my topic will help others in the future, if they came to a cross.

Basically im Idiot as before I had my X reference point set to -200, because I like move table after each operation to middle and front to easier screw and unscrew parts.
After my rebuild, I moved limit/home switch to left side of the table and G28 reference point as I call that at end of the program could not go to -200!
I've set it to 0 and I have no problem now.

[martyscncgarage]

You are not an idiot. You are no different than the rest of us working through conversions!

So you are good to go?

[Martin Zarnay]

Im good to go